Hi there,

I was wondering if any of you guys have ever used CFD to analyze wind turbine rotor performance or validate rotor design.

I am in the process of designing a set of rotor with the help of the software CFdesign. For each rotor CAD model, I can calculate the moment of inertia about the axis of rotation in the CAD, and use one of the function tools in CFdesign to let the rotor start spinning up from rest at a given wind speed, and try to pin point the equilibrium RPM of the rotor so that I can evaluate the power generation capability of that particular rotor design.

Since this is a brad new design, I have no idea what that equilibrium RPM is going to be. Based on the analyses I have run, convergent solutions are obtained with satisfactory convergence criteria met after for exmample 500 iterations. However, at I = 500, it is also observed that while this solution is considered converged and valid, the solution indicates the equilibrium RPM has not be reached, and it is likely it will take probably three to four thousands more iterations before an equilibrium RPM can ever be reached. FYI, the time step size for producing the above mentioned convergent solution is of the order of 3e-4, which means that at I = 500, total time is only 0.3 sec. I am aware that physically a rotor will not reach equilibrium RPM in 0.3 seconds.

My qeustions to the wind turbine experts are:

1) From the solution in CFdeisgn, the torque vs time curve is extracted. Power = torque * 2*pi*(rev/s), and Cp = power/(0.5*density*U^3*Area), and this is how I calculate the power absorbed by the rotor at any given wind speed and compare this with the theoretical Cp max of 0.5926 and conclude if the rotor design is good or not. Is this the right methodology?

2) To determine rotor performance, do I need to run the CFD all the way to the equilibrium RPM and use the torque value at the quilibrium RPM to do the above calculation?

3) If (2) is not neccessary, then can I use the converged RPM and torque (not at equilibrium RPM) to calculate the Cp and validate the design of the rotor this way?

Thanks for the help

Ken

Ken

This is a good question: I was thinking about this a while back.

If you wish to work out the power output from a new design of rotor then you often don't know what the optimum RPM will be. If you solve it as a steady state problem i.e. model one blade with periodic boundary conditions and solve it in a rotating frame of reference, you need to specify the rotational speed! I think the only way to do this using this method, is to run a series of simulations at various RPM's and plot the power output to find the optimum.

Keep me posted on how you get on.

Regards James

Hi James,

So what you are suggesting is to analyze wind turbine rotor just like the way of analyzing engine propeller, i.e. primarily finding out what the torque, power are at a given RPM setting.

If I read you correctly (and please correct me if I am wrong and I am throwing in some numbers here), let say for a 1.5 ft diamater engine prop, by setting a RPM of 1,500 (which corresponds to a tip Mach number of 0.10 or a wind turbine roor tip speed ratio of 3.59) with a forward speed of 10 m/s, I for example got a torque of 0.2 ft-lbf, this translate to a power of 31.41 ft-lbf/s (or 42.65 W). Now I am treating it as a wind turbine rotor. At a wind speed of 10m/s, the rotor will generate 42.65 W of power when it is turning at 1,500 RPM.

Is this basically what you are saying?

Thanks for the time. Ken

Ken

Yep, that's correct. It's more of an indirect method, since you will have to run a few different cases in order to find the peak in the power curve. I'm sure you could do a full transient simulation where you ramp up the RPM and measure the power, but this will require a full 3D blade geometry and lots of time steps. At least with the steady state rotational frame of reference method you only need to model one blade in a non-transient manner.

Are you doing this simulation as a research project or as part of an industrial investigation? There are a few papers on the web which discuss the CFD simulation of Horizontal Axis Wind Turbines (HAWT).

Regards

James

Hi James,

Thanks for the references on the papers on the web. This is an industrial investigation on new kind of wind turbine rotor (compared to the conventional 3-bladed rotor), so even myself don't really know how its performance is, even by blade element momentum technique, and therefore I am doing a first degree comparison on different rotor design by CFD.

Thanks for your help. I will keep you posted with new result.

Ken

Ken

Sounds really interesting. I've been working on a similar project, but for a tidal turbine design here in the U.K. We have conducted BEM, CFD and model testing to determine the performance of our device. I would be interested in knowing how your CFD predictions come along.

Regards

James

Hi James,

It is really good to have found someone working on similar projects and get to exchange thoughts.

What CFD software you are using? Is it one of the big three (fluent, cfx, or starcd)?

Since we are working on similar project, I was wondering if you could tell me for each of your analysis, what is your turnaround time, how big is your file (in terms of node count)?

I only have one P4 3 GHz machine (duo processors) with 4 GB of ram. This is my hardware capability. Due to this limitation, sometimes, I don't even go through the complete process of mesh dependancy studies. And for CFdesign, sometimes, when i make my mesh finer, I don't see the solution (keeping everything else constant) gradually converge to a certain point. This is the most frustating part for me.

As with the accuracy of the solution, therefore right now I think I will be only looking at relative comparison between analyses and not expect too much for absolute comparison with any experimental data.

Have you encountered the same type of problems I am facing now?

Ken

Yeah, it's good to know someone else is encountering the same problems!

We solved our turbine problem using CFX-5.7. We created a hybrid grid around on of the blades using periodic boundary conditions. A hex grid around the blade and wake, filling the remaining domain with tetra. We then solved the flow in a rotating frame of reference at the required RPM. The mesh was approx 5,000,000 nodes. It solved in ~8 hours on 30 nodes (although it was poorly parallelised). The power prediction was reasonably good but the pitching moment was very poor and good convergence was hard to reach.

Regards James

James and Ken,

I'm about to start a CFD analysis on a wind turbine blade, almost certainly a standard NACA profile, when I go back to uni at the start of the new term, using Fluent. At the moment I'm just doing as much research as I can now to reduce the time I need to bother our academics when I get going. It's for a v large offshore HAWT (3-5MW) design project forming a part of my 3rd year.

At the moment I guess I don't have much to add to your discussion, apart from adding my name to those "out there" trying this. I'll keep checking this forum, and if you're still posting I'll try and contribute with my twopence.

Yours,

Tom

Hi Tom,

Welcome to the club.

James,

So jealous of your hardware capability (30 computers in parellel). When you said you have poor convergence, what level of convergence do you have (1e-3 or higher)?

Ken

Ken

It sounds impressive, but we actually farmed out the solution of this problem to a third party. We only usually run a two node parallel solve cluster where I work at the moment.

The convergence was 1e-2 Max and 1e-4 RMS, this is very unsatisfactory in my opinion. I would have liked to have got to the bottom of this, but the project did not allow. Although the convergence is poor the predicted power seemed to be reasonably close to that found using BEM. In order to get accurate pitching moments the convergence would need to be a lot tighter, I believe.

Ken are you able to let us know a little bit more about your project?

What sort of mesh are you putting around your blade?

Regards James

Hi James,

This rotor of mine doesn't look anyway close to a conventional horizontal axis 3 bladed wind turbine rotor at all. I don't know how to describe it in words, unless i send you a JPEG (interested? let me know). Right now, I just want to know what is its power generation capability. As i know more and more about the aerodyanmics of wind turbine rotor, I am trying out different twist distribution, chord etc.(different CAD input parameters) and compare the Cp of different designs at various tip speed ratio.

So far the result indicates as tip speed ratio (X)gradually rises, Cp increases, which is good, but Cp dros from peak past tip speed ratio of 4.50, unlike typical Cp vs X plot where Cp is still about 0.50 at X > 4.0. So there must be lots of region where there is no torque generated.

In CFdesign, I can only lay out unstructured mesh. And due to hardware limitation my mesh density on the blade is no way close to the mesh density people normally see on a 2-D airfoil test. I know this impacts the solution, but from mesh dependency test, my error doesn't go significantly lower with a finer mesh, and lots of time, with more mesh, residuals (either RMS or average) are higher. The most frustating part of the program is I don't know which node generates the largest error and therefore i don't know which part in the domain I should make my mesh finer, CFdesign in this aspect sucks. Is this only happening in CFdesign, or in CFX you don't know which location (or where the node is) has the largest error too? The more I wrote about this, the more angry i am feeling.

Maybe with your experience you could give me some hints on what types of CFD analysis flow scheme will best suit this type of analysis.

By the way, I just thought of one quick question. When I am running my cases, the only this included is the rotor, and no nacelle and tower. What I am seeing on axial velocity flow field is directly downstream of the rotor along the X-axis (r/D = 0, X/D = 2 - 4), the axial velocity is really low (upstream windspeed of 10 m/s), even negative (flow reversal). Have you ever visuallize this type of flow field phenomenum?

Based on momentum theory, the stream tube expands past rotor, and I am seeing that but the axial velocity should not decrease by so much to the extend of "generating" a flow reversal zone, right?

Ken

Ken

Sounds like you've done quite a lot of work. I guess the tetra mesh is the quickest way of meshing your geometry, but a hex mesh would definitely give you better results. If you can't do a full hex mesh then just do a hybrid mesh, with a hex mesh around the blade and into the wake and a tetra mesh filling the rest of the domain.

The flow reversal downstream of the blade disk does sound strange, i would expect the flow to be slower but not reversing!

With regard to the location of maximum residual CFX-5.7 allows you to find this out quiet easily.

James

James and Ken I'm also doing a CFD analysis on a wind turbine blades.My software is Fluent.My method is what you mentioned formerly,and as a steady state problem i.e. model one blade with periodic boundary conditions and solve it in a rotating frame of reference.My wind turbine has two blades and diamater is 1.16m.I set a RPM of 368 with a forward speed of 5.6m/s. Total mesh is 500,000 elements.The boundary conditions is uniform inlet velocity,pressure outlet and pressure far field of the cylindrical domain.The turbulence model is k-¦Ø SST. But the power predition is largely lower than experiment data and reach convergence quickly with one hour or less than one hour. Could you help me analyse why the power prediction is lower ? Could you give me a few papers which diacuss the CFD simulation of Horizontal Axis Wind Turbine (HAWT).

Thanks for the help

ruibo

Hi Ruibo,

Good to know that someone else is also doing CFD work on wind turbine rotor. First of all, what type of convergence criteria you have on your results? Is the result you mentioned already the final product through mesh dependency test? Based on the 500k node counts my guess is yes, right?

Secondly, you must have impressive hardware capability, only 1 hr of runtime for each analysis with 500k nodes, impresive! By the way, how big is your cylindrical domain?

I don't know how the final result, power is extracted from Fluent, is that number coming from one torque number (already internally calculated by Fluent) or you made a few spanwise cut on calculated sectional torque, than intergrating the numbers to get to the final torque value? If you happen to have experimental results on sectional torque, compare between the experimental and your computational results and find out which span location gives you the maximum discrepancy and work from there. Maybe at certain region or span location mesh is not fine enough? Or have you tried out different turbulence model? Why did you pick K-(can't read) SST model at the first place? Any papers mention this is good for this kind of flow problem, or this is reconmended by Fluent tech support guy? So far I still haven't found any good papers on HAWT papers. You might want to check out some papers on CFD analysis on propeller blades, that might help also, i hope.

Good luck, keep in touch.

Ken

Hi James, thanks for the reply. In fact I have been wanting to switch from CFdesign to either CFX or Fluent, but my company is just neither big enough nor have that much of a cash flow to buy either Fluent or CFX. I think that's the way it is. As i mentioned before, for the results I am getting, I am only confident in the relative comparison among different models but not absolute comparison between computational and experimental results. Well, the later part of my project is to build some prototypes and stick them in the windtunnel. Then I will definitely have a feel on what performance the rotor really has. Thanks for your help, really appreciate it.

Ken

[johnstewart00]

Hi,
I am having trouble validating a mesh for an airfoil created in gambit.

The air speed is 50m/s, set in fluent at the inlet.(left)
The height of each cell is 0.00038. not sure of the units.

Any help would be very much appreciated because I am at a stand still with my project at the moment

Thanks,
John

[sivarama1]

Hi all,
any body know,i am first time analyzing wind rotor,how to start,how to mesh,any body give clarifications,
But i know how to analysis steam turbine blades.
Thankyou

[vanni]

Hello guys,

I want to study a new wind turbine with vertical rotational axis.
I think, on the base of the shape of the rotor, that a sliding/dinamic mesh is necessary and I would like to start with a 2D simulation.

Obviously I don’t know the rotational velocity of the rotor at a specific wind velocity.
I think that I must take into account the torque and power necessary to generate electrical energy.

The question is: how can I setup this simulation? How can I make the flow to move the rotor?

I think to use this formulation for angular velocity ω that must be applied to moving/sliding mesh (that is to the blades) by an user defined function.

ω t = ωt-1 + [Maer t-1 - M res (ωt-1)] / Irotor * Δt

where:

Maer= torque calculated on rotor due to flow
Mres(ω) = function for torque due to electrical energy power generation depending on ω itself.
Irotor = rotor Inertia

Do you agree?

Thanks in advance
vanni

[sharan]

Hi,

I am doing flow anlysis on a Rotor of 2.1m arm length (4.2m span) using CFX to find the power required to rotate it at 1500 rpm (this corresponds to Mach 1 at the tip of the rotor).

The root thickness is 0.03m and the tip thickness is 0.012m. Root chord is 0.45m and tip chord is 0.12m.

After doing a run using CFX the torque measured using the monitors option is 5000 n-m (to my surprise). With this torque the power required will be very high.

Power = torque * omega = 5000*157.4
Power = 1053 HP

which is much more than the expected value.

I used all the default settings in CFX for doing the meshing and analysis and choosen the rotating domain with 1500 rpm. The fluid is choosen as Air at 25 degrees C.

As expected the Mach number near the tip is coming close to 1.

Can anyone suggest me a better approach to the problem.